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SolidWorks Sketch Tools Through a Disc Brake Sketch
A free lesson from Skill-Lync's Mold Design using SOLIDWORKS course, on Grow by Skill-Lync · Last updated 16 Nov 2026 · Session: “SolidWorks Sketching Tutorial : Disc Brake Sketch”
What will you learn in this free Mold Design using SOLIDWORKS lesson?
The instructor builds a disc brake sketch on the front plane using the circle, smart dimension, straight slot, three-point arc and circular pattern commands. The lesson dimensions concentric circles of 30, 125 and 175 mm, adds relations, and patterns 20 slots and 7 arc cuts until the sketch is fully defined.
- Circle and smart dimension commands
- Adding vertical and coincident relations
- Straight slot and three-point arc tools
- Circular sketch pattern and fully defined sketches
What comes after lesson 3?
Later in Skill-Lync's Mold Design using SOLIDWORKS course (paid): lesson 4, Sketching Tools Tutorial Series - Telephone Handset Sketch; lesson 5, Sketching Tools Tutorial Series: Creating a Fidget Spinner; lesson 6, Sketching Tools Series: Plumber Block. The full course has 41 lessons (14 h 11 min of video); see the course overview or its price and syllabus.
Lesson transcript
Machine transcript of the lesson audio (lightly cleaned). Technical terms may contain errors; the video is the reference.
Hello guys, welcome to the first SOLIDWORKS sketching tutorial video. I am planning to have 4 sketching tutorial videos and in each video I will be making a sketch that will make use of multiple sketching tools. After watching these 4 videos, I hope that you will be able to make any sketch that you might require during the mold design process. If you want, you can try recreating the sketches that I make in these videos or if you are confident that you have understood all the tools, then you can directly start working on the assignments.
In the first video, I will be explaining how to make a sketch for the disk break. So before starting the sketch, make sure that you are in the sketch mode. The option which is currently active will have a white background and you can see the other options will have a grey background. And above that you have the command manager where you can see all the commands that are available in the sketch tools. So this is the disk break sketch that we will be making in this video. In order to make this sketch, I will be using the circle, smart dimension, slot, circular pattern, and the three point arc commands.
So the first step is creating the circles for the disk break. So for creating the circles, I will be using the circle command and then using smart dimension command, I will assign correct dimensions to the circle. Now we will start creating our sketch in SOLIDWORKS. So to start creating any sketch, you will first have to select the plane on which you want to create the sketch. Here I will be sketching on the front plane. So for that, I will have to click on the front plane in the feature manager and then I will click on the sketch option.
Now we can start creating the sketch which you see in the image. You can see that we need to make three circles first. So I will go to the circle command in the command manager. If I click on the arrow next to the circle command, you can see that we have two options here, circle and perimeter circle. If you select the circle option, then you will have to specify the center and the radius of the circle. And if you select the perimeter circle, then you will have to select three points that define a circle.
So here I will go with the circle command. I will select the origin as the center and then left click at some distance. And you can see a preview of a circle that will be formed. On the left under options, you can see a for construction option. If you click on this, then you can see that you get a construction line. So if you want to create construction lines, you can use this. But since I don't want a construction line here, I will untick this option.
So to exit the command, you can either press the escape key or click on the green tick mark on the left. Now you can see that a circle has been formed. Now I will repeat the same process to create two more circles. I am selecting the center as the origin for all the circles so that circles formed are concentric. Now we will assign dimensions to this circle. So for that, I will click on the smart dimension command in the command manager. And then I will click on the innermost circle.
Move your mouse cursor. And now if you left click, then you will get an option to specify the dimension. Here I can type 30 since I want the innermost circle to be 30 mm. And then click on the green tick mark. And now you can see that the dimension is assigned. You will also notice that the innermost circle is black in color and the other circles are blue in color. The black color represents that the sketch is fully defined and the blue color shows that the sketch is not fully defined.
Now I will proceed to give dimensions to the other two circles. So I will select the middle circle and give it a diameter of 125. And I will give the outermost circle a diameter of 175. Now let's say you accidentally assign a wrong dimension to a part. Then to edit the dimension, you can just left click on the assign dimension again. And then assign some new value. The second step is the creation of the slot. We will be using the straight slot command to create the slot as shown in the diagram.
And then we will define the slot by giving proper dimensions. I will click on the slot command in the command manager. On the left under the slot types, you can see four types of slots. The top two are the straight slots and the bottom two are the curved slots. The only difference between the top two types is the selection of the points for making the slots. You can create the same slots using either of the options. I will be selecting the first option which is a straight slot.
And then I will select the two endpoints and the radius for the slot. Now I want the center of the slot and the origin to be on the same vertical axis. So for that, I will have to define a relation between the origin and the center of the slot. For defining a relation between points, click on the slot center, press and hold ctrl key and then select origin. And after selecting the second point, you will have a properties box on the left. In the bottom of the box, you have the add relations option where you can select the relation you want between these two points.
Since I want these points to be on the same vertical line, I will select the vertical relation and then click on OK. Now both the points are in the same vertical line. Similarly, you can add multiple relations such as horizontal, coincident, concentric, tangent, etc. by selecting multiple points, lines or arcs. Now I will give dimensions to the slot. First, I will specify the distance between the center of the slot and the circle center as 75 mm. Then I would like to specify the angle of the slot as 45 degree.
Now to specify the angle, I need a reference line with respect to which the slot is 45 degrees. So I can either create a new line or I can just select the top plane and the edge of the slot and give the angle as 45 degrees. Now I will define the length of the slot. So I will select this edge and then give it a distance of 10 mm. And then I will select the arc and give it a radius of 2.25. Now I want to create multiple copies of the slot throughout the entire circle.
For that, I can either create multiple slots or I can directly use the circular pattern command to make multiple copies of the slot around the circle. After using the circular pattern, your sketch should look like the diagram on the right. So for selecting the circular pattern option, go to the linear sketch pattern and click on the arrow next to it. Now you will have two options. The linear sketch pattern is used to make multiple copies along a straight line. And the circular sketch pattern is used to make multiple copies along an arc.
Since in this case, we want multiple copies along an arc, I am going to select the circular pattern option. On the left, the first option which you have is selecting the center of rotation. For that, I am going to select the center of the circle. And here you will get an option, entities to pattern. Here you can specify the entity which you want to copy. So since I want to copy the slot, I will select the slot as the entity to pattern. Now you will see a preview of the pattern that will be generated.
On the left, we also have a spacing option. Here you can specify the angle in which you want the entities to be patterned. Since I want the pattern throughout the entire circle, which is 360 degrees, I will keep this value as it is. And below that, you have the option to specify the number of instances. Since it is on 4 currently, we have 4 slots in the preview. I want to increase the number of slots. So I will change this value to 20. And now you can see the preview of multiple slots.
I am going to click on OK and the pattern will be generated. Now you can see that the pattern entities are not fully defined as they are blue in color. If I left click on the center of any slot, hold and drag it, you can see that it is free to move. So to fully define the sketch, I am going to add another relation. I will select the center of the pattern and then I will select the origin and add a coincident relation. Now you can see the sketch is fully defined.
Now we will be making some additional cuts in the disk break. For making the sketch, I will be using the 3-point arc command and then I will add dimensions to fully define the sketch. And after fully defining the sketch, we will use the circular pattern command again to make multiple copies of the cut around the circle. Now I will go to the 3-point arc option in the command manager. If I click on the arrow next to it, you can see three options. The center point arc and the 3-point arc option are similar to the circle and the perimeter circle option.
The only difference is we create arcs instead of whole circles using this command. For now, I will select the 3-point arc option and sketch a few arcs. So for the 3-point arc, you first select two endpoints and then select a point which defines the radius of the arc. I will repeat the same process and make two more arcs. Now I want the 4th arc to be tangent to the two adjacent arcs. For that, I can either create a 3-point arc and then add tangent relation between the arcs.
Or I can directly select the tangent arc option and then select the two points. So the arc that is created is tangent to the two adjacent arcs. Now I will add dimensions to the sketch to fully define it. Now as the sketch is fully defined, I will use the circular pattern command again to create multiple copies of this entity around the circle. So I will click on the circular pattern and then I will again specify the center of the circle as the point of rotation. I will select the arcs which I made as the entities to pattern and I will specify the number of instances as 7 and then click on OK.
The pattern will be created. Now to fully define the sketch, you can again drag the pattern out a little and then give coincident relation to the center of the pattern and the origin. After this step, the sketch should be fully defined and with this, we have completed the disk break sketch. So in this session, we created the disk break sketch. We learned how to use the circle, smart dimension, slot, circular pattern and the three-point arc commands while creating the disk break. And that's it for this session.
Thank you for watching the video.